Rotor dynamic analysis with superelements (SOL 414,103)

SOL 414,103 Eigenvalues and Superelement Reduction provides you with computation options for the following:

• Eigenvalue analysis

• Superelement reduction

In the superelement reduction analysis, SOL 414,103 Eigenvalues and Superelement Reduction condenses a rotating part to its stiffness, damping, and gyroscopic matrices at specified retained nodes. After you create the superelement of the rotating part, you can use it to replace an actual rotor in a full assembly model. Because the superelement is a reduced representation of the rotor, the overall solve time in the full assembly is reduced.

You can also use SOL 414,103 Eigenvalues and Superelement Reduction to generate superelements of superelements when you want to decrease the number of retained nodes. The model in which you use the superelements can contain multiple occurrences of the same superelement as well as multiple unique rotor superelements. Also, if the model in which you plan to use the rotor superelement is in a different unit system than the unit system in which the superelement was created, you can select the unit system of the original model when you add the superelement to the assembly FEM file. You can use the rotor superelements in all of the SOL 414 solution types except for SOL 414,101 Maneuvers. SOL 414 takes the units conversion into account.

The generated rotor superelement is stored in the Samcef .sdb and .u18 files with the following file names:

• sessionname_solutionname.sdb

• sessionname_solutionname.u18

Note:

In Simcenter Nastran SOL 103 analyses, the superelements for non-rotating parts are created in the standard .op2 format. Only rotor superelements generated by SOL 414,103 are created in the Simcenter Samcef .sdb format.

2D axisymmetric FEM model	2D axisymmetric superelement with boundary nodes

In addition to generating superelements for rotors, you can also perform an eigenvalue analysis.

SOL 414,103 eigenvalue analysis

SOL 414,103 with the Eigenvalues option is similar to a SOL 103 Real Eigenvalues solution. Use it to generate a modal analysis of the model at rest with no rotating parts. You can use the eigenvalue analysis with 1D, 2D, 2D axisymmetric, 3D, 3D cyclic symmetry, and combined 2D axisymmetric and 3D cyclic symmetry models.

When you create a SOL 414,103 eigenvalue analysis, you can:

• Add one of the following optional preload subcases:Subcase - Static Loads****Subcase - Transient PreloadNote: The preload subcase is always exported as the first subcase in the solution even if it appears below Subcase - Eigenvalues and Superelement in the Simulation Navigator. You can visually position the preload subcase first when you add it to the solution by setting the Relative Position list to [Before] Subcase - Eigenvalues and Superelement in the Solution Step dialog box.

• Generate either real modes or complex modes.

• Define damping in the same ways that you can in the other SOL 414 solution types.

Note:

If your model contains CBEAR elements that are collected in a group that you select when you create the rotor region, we recommended that you change those bearings to CBEAR2 elements. Otherwise, CBEAR elements are not taken into account because SOL 414,103 eigenvalue analysis is solved without any rotor definition.

SOL 414,103 superelement analysis

SOL 414,103 with the Superelement Reduction option is similar to a SOL 103 Superelement solution, but in addition to creating a condensed model (stiffness, damping, mass matrices), SOL 414,103 with the Superelement Reduction option takes rotation into account. Use it to create superelements of the following:

• 3D model of a rotor

• 2D axisymmetric model of a rotor with Fourier harmonics

• 1D model of a rotor

You can add one of the following optional preload subcases to the superelement analysis:

• Subcase - Static Loads

• Subcase - Transient Preload

Note:

The preload subcase is always exported as the first subcase in the solution even if it appears below Subcase - Eigenvalues and Superelement in the Simulation Navigator. You can visually position the preload subcase first when you add it to the solution by setting the Relative Position list to [Before] Subcase - Eigenvalues and Superelement in the Solution Step dialog box.

For more information on creating rotor superelements, see Modeling considerations and best practices for defining rotor superelements next in this topic.

Modeling considerations and best practices for defining rotor superelements

The following parameters must be consistent between the solution that creates the superelement and the solution that uses the superelement:

• Nodes to retain

• Eigenvalues

• Reference frame

• Coordinate system

In addition to ensuring consistent modeling in the superelement generation analysis and the final analysis, a best practice is to validate the superelement results.

Defining the nodes to retain

The retained nodes are important because they are the nodes that you can use on the generated superelement when you add the superelement to an assembly FEM file. You define retained nodes at the locations where you want to create bearing and bushing connections, apply boundary conditions and forces, and monitor and request output.

Retained nodes in a 2D axisymmetric rotor for (1) Fixed Boundary Degrees of Freedom (orange) and (2) Free Boundary Degrees of Freedom (green)

Retained nodes in the superelement rotor before adding bearing connections and boundary conditions

To create a retained node, select a node on the rotor and apply the Fixed Boundary Degrees of Freedom or Free Boundary Degrees of Freedom constraint, as follows:

• For nodes to which you will apply boundary conditions, including a constrained node in a bearing connection, apply the Fixed Boundary Degrees of Freedom constraint.

• For nodes to which you will apply loads (such as unbalance and forces), bearing connections between different parts of the rotating part (such as the rotors or rotor-stators), monitoring, and output requests, apply the Free Boundary Degrees of Freedom constraint.Monitoring of output using the Report simulation object is supported in SOL 414,111 harmonic response analysis or SOL 414,129 transient response analysis.

Note:

At a minimum, create one retained node for each bearing, force load, boundary condition, output request, and monitor.

Requesting too many modes in relationship to the number of retained nodes can yield redundant static and normal modes with singular stiffness matrices, which can cause the size of the rotor superelement to be larger than the rotor model.

Specifying boundary degrees of freedom

SOL 414,103 superelement generates a component mode synthesis reduction to represent the component's dynamic behavior of a rotating component. You use sets to define degrees of freedom for the boundary where the component is connected to other components in the structure. The boundary degrees of freedom can be fixed or free.

• Define the fixed boundary degrees of freedom using the Fixed Boundary Degrees of Freedom constraint (BNDFIX or BSET).

• Define the free boundary degrees of freedom using theFree Boundary Degrees of Freedom constraint (BNDFREE or CSET).

Specifying eigenvalues

You can specify only real modes, not complex modes when you create the superelement. When you specify the upper limit for the Real Eigenvalue – Lanczos modeling object for the superelement, set the highest frequency of the superelement rotor to twice the highest frequency of the original rotor.

For example, if the original rotor rotates from 0–6,000 rpm, 100 Hz is the highest frequency of the analysis. Therefore, in SOL 414,103 Eigenvalues and Superelement Reduction, set the highest frequency of the Real Eigenvalue – Lanczos modeling object to 200 Hz.

To avoid bad matrix conditioning, ensure that the number of modes you request is not set too high. For example, 20 modes for a 1D rotor is typically sufficient.

Setting the reference frame and applying damping

You must use the same type of reference frame (fixed or rotating) for the creation of the superelement and the analysis of the superelement.

You can set Rayleigh (viscous) or structural (hysteretic) damping, as well as overall structural damping and element structural damping. However, you can omit damping when you generate the superelement and instead apply viscous or hysteretic damping on the FE Model Component Representation dialog box when you replace a component FEM file with the rotor superelement. If you want to apply damping, do one of the following:

• If you create a superelement in a fixed reference frame, apply damping when you create the superelement.

• If you create a superelement in a rotating reference frame, for example, if your rotor is non-symmetric, apply damping in the analysis that uses the superelement and not when you create the superelement.

When you create a superelement with a rotating reference frame and you specify a static or transient preload with centrifugal loads using the Rotation (RFORCE) command, you do not have to define the static or transient preload again when you add the superelement to the model. The preload is already taken into account when the superelement is generated.

• If you use an angular velocity of 1 rad/s in the static preload, the current rotor speed is used in the computation of the centrifugal loads.

• If you use an angular velocity other than 1 rad/s in the static preload, the superelement is valid for that speed only.

The bearing coefficients must be isotropic, which is the same as for any calculation in the rotating reference frame.

You set the reference frame for SOL 414,103 superelement analysis in the Solution dialog box on the Bulk Data page by selecting FIX or ROT from the Reference System list.

Specifying rotor speeds

The eigenvalue analysis is performed for a rotor at rest, so rotor speed is not needed. Specifying the rotor speed for the superelement analysis depends on the type of reference frame.

• Fixed reference frame—The rotor speed is taken into account when the superelement is used in an analysis. Thus, you do not specify a rotor speed in the superelement analysis.

• Rotating reference frame—You can specify a rotor speed, or you can use the rotor speed that is set in the analysis that uses the superelement. In the Rotation load:To specify a rotor speed, set Angular Velocity to a value other than 1. When you do this, the superelement is valid for this rotor speed only.To use the rotor speed of the analysis that uses the superelement, set Angular Velocity to 1 rad/s.

Setting the coordinate system of the superelement

The coordinate system of the original rotor and the superelement rotor must be consistent. The Z-axis of a rotor always defines the direction of rotation of the rotor. Therefore, when you add a superelement to an assembly, the new rotor region (created with the retained nodes of that superelement) must have the same local Z-axis as the original model.

Validating the generated superelement

Validation lets you compare the results from the original model and its superelement representation. If the results are very similar, the superelement is an adequate representation of the original part.

We recommend that you perform the following comparisons to validate the quality of the superelement.

• Using the original model with connection elements and boundary conditions, create and solve the following solutions:SOL 414,103 eigenvalue analysisSOL 414,110 complex modal analysis with the rotation speed set to 0The results of both solutions should provide the same modes.

• Using the original model in another model configuration (for example, no boundary conditions, no connection elements, and so on), create and solve the following solutions:SOL 414,103 superelement reduction analysisSOL 414,103 eigenvalue analysisThe results of both solutions should provide the same modes.

• Use the superelement in the same configuration as the original model (for example, use the same forces, same connection elements, and so on). The results of the solution for both models should be very similar.

Post-processing rotor dynamic superelement results

When you post-process results for an analysis that uses a superelement, the superelement is represented by its retained nodes in the graphics window. However, you can restore the superelement to the original model using the Superelement Recovery command.

You can recover superelement results for SOL 414,103, SOL 414,110, SOL 414,111, and SOL 414,129 rotor dynamic analyses.

Frequency results for superelement generated from a 3D model	Modal results for recovered superelement for the same 3D model

Where do I find it?

Creating SOL 414,103 Eigenvalues and Superelement Reduction

Application	Pre/Post
Prerequisites	A Simulation file as the work part and displayed partSimcenter Nastran as the specified solverRotor Dynamics as the specified analysis typeSOL 414,103 Eigenvalues and Superelement Reduction as the specified solution typeEigenvalues or Superelement Reduction as the specified computation option
Command Finder	Solution

Using superelement representations in SOL 414 analyses

Application	Pre/Post
Prerequisites	An assembly FEM file as the work part and displayed partSimcenter Nastran as the specified solverRotor Dynamics as the specified analysis typeAny of the following as the specified solution type:SOL 414,103 Eigenvalues and Superelement ReductionSOL 414,110 Complex Modal AnalysisSOL 414,111 Harmonic Response****SOL 414,129 Transient ResponseResults for SOL 414,103 Eigenvalues and Superelement Reduction that generated a superelement
Simulation Navigator	Right-click a component FEM→Edit Representation
Location in dialog box	FE Model Component Representation dialog box→Representation list→Nastran Rotor Super Element

Recovering superelements in post-processing

Application	Pre/Post
Prerequisites	A Simulation file as the work part and displayed partSimcenter Nastran as the specified solverRotor Dynamics as the specified analysis typeAny of the following as the specified solution typeSOL 414,103SOL 414,110SOL 414,111SOL 414,129Results for a solution that uses superelements
Command Finder	Superelement Recovery (Rotor Dynamics ribbon bar)

Rotor dynamic analysis with superelements (SOL 414,103), Simcenter 3D 2021.1 Series

© 2020 Siemens

window.mainLanguage="en_US"

window.delivId=""

window.projectId=""

MathJax.Hub.Config({ TeX: { extensions: ["autoload-all.js"] }, tex2jax: { displayMath: [ ] }, "SVG": { scale: 125 } });